HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

Results 1 to 9 of 9

Thread: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

  1. #1
    Member okuma1984's Avatar
    Join Date
    Oct 2018
    Location
    TILSONBURGE
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    Hi there I am wondering if anyone knows how to set the machine in metric?? G20 to G21 ?? ? ? I know that's Fanuc but does Okuma work like that too? or do you convert to inches?


    I have done several threading jobs with this machine in inches however I am having a hard time writing Metric or converting it in Okuma


    so basically I am trying to 9MM x 1.25 pitch

    can anyone write a G71 line or tell me what to fill in the blanks in IGF?

    major diameter 9mm
    minor 7.647mm
    pitch 1.25mm
    Lead?
    TPI??
    X Start .38"
    X finish or minor diameter .301"
    H[eight of thread]: .0266 I believe ? (or 9 - 7.647 /2 in MM)

    that's all I got for now.

    thanks

    Similar Threads:
    Attached Thumbnails Attached Thumbnails HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP-img-1989-jpg  


  2. #2
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3656
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    Convert pitch to Imperial
    1.25 / 25.4=0.0492

    Calc TPI
    1 / 0.0492=20.32

    The lead is 0.0492'', the TPI is 20.32

    Major dia = 0.354''

    0.866 is a constant for metric thread depth
    0.866*pitch = 0.866*1.25 = 1.0825mm = 0.0426'' thread depth
    0.0426*2 = 0.0852''
    0.354-0.0852=0.2687''

    Minor dia = 0.2687''

    This should give you enough to set it up just like cutting Imperial threads.

    Jim Dawson
    Sandy, Oregon, USA


  3. #3
    Member okuma1984's Avatar
    Join Date
    Oct 2018
    Location
    TILSONBURGE
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    Quote Originally Posted by Jim Dawson View Post
    Convert pitch to Imperial
    1.25 / 25.4=0.0492

    Calc TPI
    1 / 0.0492=20.32

    The lead is 0.0492'', the TPI is 20.32

    Major dia = 0.354''

    0.866 is a constant for metric thread depth
    0.866*pitch = 0.866*1.25 = 1.0825mm = 0.0426'' thread depth
    0.0426*2 = 0.0852''
    0.354-0.0852=0.2687''

    Minor dia = 0.2687''

    This should give you enough to set it up just like cutting Imperial threads.
    thanks a lot, Jim. so provided all that
    g50s200
    T20202
    G95
    G97S100M3
    G90G1X.38Z.1F50.
    G71X.2687Z-1. H.0426 (D..005?) F.0492 (U.001?) M73M34
    G80
    yeah?


    do you use M33 or M34? which is better? is it just preference?
    I am putting threads on an already hardened 3/8" bolt. I bought a long one so I could cut it off and put threads on the end of it.

    sorry if this is confusing

    Last edited by okuma1984; 07-07-2019 at 10:53 PM.


  4. #4
    Member okuma1984's Avatar
    Join Date
    Oct 2018
    Location
    TILSONBURGE
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    is everything here radial ?? and no J value I take it since it's Metric ?or J is # of threads per inch
    and we figured it's 20.33? does the machine like decimals?



  5. #5
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3656
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    Does your machine have a G32 threading cycle available? That's what I use.

    I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

    - - - Updated - - -

    Does your machine have a G32 threading cycle available? That's what I use.

    I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

    Jim Dawson
    Sandy, Oregon, USA


  6. #6
    Member okuma1984's Avatar
    Join Date
    Oct 2018
    Location
    TILSONBURGE
    Posts
    21
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    Quote Originally Posted by Jim Dawson View Post
    Does your machine have a G32 threading cycle available? That's what I use.

    I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.

    - - - Updated - - -

    Does your machine have a G32 threading cycle available? That's what I use.

    I normally set up the M33 or M34 in the CAM program and let it sort that out. In Fusion there is an option switch for this.
    I think I tired it once but not G32
    I tried G33 which is like G92 in faunc correct? I tried G33 but the control doesn't like it. so I have been working with G71 instead.
    G33 X Z F J M23
    X
    X
    X
    ..
    seems pretty easy

    but anyway where in IGF is M34 or M33 determined? and if you noticed in my picture spinning clockwise is written as M41 .. .
    why?



  7. #7
    Member Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    3656
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    According to my list, the M41 is Spindle Gear Range 1, but I don't see a M3 (Spindle CW) or M4 (Spindle CCW) on your picture which is a bit odd. But understand I am no expert on Okuma or Fanuc for that matter. G33 (Fixed thread cutting cycle) by the description seems like a G32, but I'm not sure. In the example code below, the idea is to make a pass everytime a G32 is commanded, with a fadeout at the end of the thread. X and Z reposition at the start of the thread for each successive pass. Conversely, G71 combines this all into one line of code using a number of parameters. As near as I can tell, the M33/M34 tells the controller to fadeout the thread at the end (or not), not sure where this is invoked. Fusion 360 has a switch to fadeout or not.


    This is a Haas turning post from Fusion 360, 9mm x 1.25 thread, 1 inch long converted to Imperial units. 5 passes with a spring pass. This will run on my lathe, but your lathe might choke on it. If you choose to try this be very careful, turn the feed and rapid way down.

    (Thread1)
    N15 T100
    N16 G99
    N17 M22
    N18 G97 S200 M3
    N19 G54
    N20 M8
    N21 G0 X1.154 Z0.1969
    N22 G1 Z0.246 F1.5748
    N23 X0.3323
    N24 G32 Z-0.9916 F0.0492
    N25 X0.3491 Z-1. F0.0492
    N26 G1 X1.154 F1.5748
    N27 Z0.246
    N28 X0.3155
    N29 G32 Z-0.9832 F0.0492
    N30 X0.3491 Z-1. F0.0492
    N31 G1 X1.154 F1.5748
    N32 Z0.246
    N33 X0.2987
    N34 G32 Z-0.9748 F0.0492
    N35 X0.3491 Z-1. F0.0492
    N36 G1 X1.154 F1.5748
    N37 Z0.246
    N38 X0.2819
    N39 G32 Z-0.9664 F0.0492
    N40 X0.3491 Z-1. F0.0492
    N41 G1 X1.154 F1.5748
    N42 Z0.246
    N43 X0.2651
    N44 G32 Z-0.958 F0.0492
    N45 X0.3491 Z-1. F0.0492
    N46 G1 X1.154 F1.5748
    N47 Z0.246
    N48 X0.2651
    N49 G32 Z-0.958 F0.0492
    N50 X0.3491 Z-1. F0.0492
    N51 G1 X1.154 F1.5748
    N52 Z0.1969

    Jim Dawson
    Sandy, Oregon, USA


  8. #8
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    3854
    Downloads
    4
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    G20 to G21 ?? ? ? I know that's Fanuc but does Okuma work like that too?
    SIAS?

    Cheers
    Roger



  9. #9
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2796
    Downloads
    0
    Uploads
    0

    Default Re: HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

    hi, you don't need to re-set the machine, to be able to deliver a metric or inch thread; you need a bit of infos about :
    ... threading cycles ( pls find attached pdf )
    ... metric threads profile iso sizes ( there are tables all over the internet )

    do you use M33 or M34? which is better?
    please look inside attached pdf, for infeed patterns; some like to use M33 M74, whatever works usually i don't bother with such patterns, unless i have a nasty thread with calls for specific attention

    is everything here radial ?? and no J value I take it since it's Metric ?or J is # of threads per inch
    you may run some trials, to figure out the answer : program something in igf, inspect the code, and see how the machine performs ( inspect coordinates ) : these should give you an answer

    also, check definition of F & J in attached doc, at page 15

    does the machine like decimals?
    about threading arguments, some programmers consider that they have to be integers ... but this is not true, at least on osp300

    I tried G33 but the control doesn't like it.
    maybe is an option for your machine, or maybe you did not write it ok ... i don't know, but i can say that i use g33 a lot

    but anyway where in IGF is M34 or M33 determined?
    i don't know for your machine ... normally, there should be a cnc parameter, or a igf parameter, but i don't know it's location for your machine

    and if you noticed in my picture spinning clockwise is written as M41 .. . why?
    since rpm is 111, with m41, 1st gear, spindle will output more torque

    but I don't see a M3 (Spindle CW) or M4 (Spindle CCW) on your picture which is a bit odd.
    it may be possible that a previous operation allready used M03, and igf 'optimizations' occur

    can anyone write a G71 line or tell me what to fill in the blanks in IGF?
    i am not near a machine right now, and even if i would, machine is in metric, so i won't be able to guarantee my code but, if you wish, i could show you how i program a 7tpi thread : G33 X Z F+25.4/7 G95

    you know, if you have futher questions, or curious about how others are doing things, there is an okuma forum, and it is pretty good : https://www.cnczone.com/forums/okuma/

    kindly

    Attached Files Attached Files
    Last edited by deadlykitten; 09-11-2019 at 10:49 AM.
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP

HOW DO YOU METRIC THREAD WITH OKUMA LATHE OSP